3D Tutorial (Solidworks)

[JorgensenSteam]

I am heck-bend on learning 3D modeling, and having a rough time with it.

I made a little headway last night with some 3D modeling concepts, and I will post the ideas I came up with in dealing with 3D here.

After several false starts, I was able to make the frame for the TB5 engine in two parts, and assemble them.

The frame is actually one piece, but I could not figure out how to do a one-piece design.

Here is what I came up with.

Pat J

 

[walnotr]

You are on the right track but you need to think more 3D. You should start by drawing the "L" shape and extrude it to the length you want. Then create additional sketches on the on the planes of the two legs of the "L" to cut extrude the additional shapes in the legs. That way you you get a solid object that doesn't have to be an assembly. SolidWorks is a very powerful program with many features you may never use but can be useful to create many intricate shapes. Keep in mind there are always many ways to attack a problem and jumping in and trying things is the best way to build your skill set. I found it helpful to build 3D models from existing 2D drawings then make the assemblies from the resulting models. Good Luck!

Steve C.

 

[coopertje]

Hi Pat,

In my little experiance with 3D I always attack the parts as if I was behind my milling machine. I start with a solid block and start to cut away material, add radius, drill holes etc. Solid works follows this way of thinking quite well. Maybe not the fastest way to draw a part but for me at least a way that I understand....

Regards Jeroen

 

[imagineering]

Hi Pat,

In my little experiance with 3D I always attack the parts as if I was behind my milling machine. I start with a solid block and start to cut away material, add radius, drill holes etc.
Regards Jeroen

I work the same way with Inventor 2011. This method also helps visualising Workflow when it comes to Milling Time.

Murray.

 

[Maryak]

BoS,

It took me a very long time to get a basic understanding of 3D. Having got this far.............. I start with a plan view of the part and extrude the Z axis into the page. In turbocad the views of the part then follow the 3rd angle projections of said part which is now a solid. From this I take the appropriate view create an outline followed by an extrusion, (again into the page), of the unwanted section then 3D subtract it from the base solid.

Hope this helps

Best Regards
Bob

 

[JorgensenSteam]

Here is an item I found at Dessault.
This helps with the visualization.

Thanks all for the feedback.

I will try the frame again, and extrude as an "L" shape into one piece.

Pat J

 

[JorgensenSteam]

Here is my second attempt at the TB5 frame, this time with an extruded one-piece "L" section.

This works better.

I think I have finally made some headway on the 3D front.
You really do have to think "milling machine", and think in 3D shapes as mentioned by Steve C and Jeroen above.

And I agree with Bob, it has taken me a long time to get my head wrapped around the 3D concepts. If it were not for the fact that so many others seem to use it with ease, I would never attempt it. It is one of those "if they can do it, so can I", but it sure has not been easy to get started.

Pat J

 

[gbritnell]

Hi Pat,
I took an apprenticeship as a metal pattenmaker many years ago. From there I went onto the 'board' as a pattern and corebox designer. All the drawing (2D) was done by hand but you had to be able to visualize the shape of a part to make sectional views.
When the company got into 3D cad modeling I had gone back to the shop to run machines. It wasn't until we purchased some CNC mills that I had the opportunity to go back to the design and draw part of the trade. They needed 2 cutterpath/CAD modelers so with my previous background I got the job.
In the 15 years that I worked with the various versions and had to help train upcoming apprentices the first thing I stressed was don't get frustrated, learn it a bit at a time. Some of the versions can be very complex with drop down menus and multitudes of strange looking icons. If a person has only worked with 2D and has never done any type of modeling before it can seem insurmountable.
Having to learn it buy yourself with no mentoring can be a daunting task but certainly not impossible. Just bite off a little at a time and before long it will fall into place.
gbritnell

 

[JorgensenSteam]

Thanks for the encouragement George.
Solidworks has some extremely powerful features, but is just different enough to throw me. I am starting to make progress though.

Here is the sequence I used for the above part. Although this is a simple part, the difficult thing was coming up with this sequence. Once you figure out the approach, then making model is easy.

For this part, I drew two lines at 90 degrees on the front sketch plane, then offset them by 0.5", and finished the sketch by closing the ends to create the "L" shape.

I then went to 3D mode (the jumping between 2D sketch mode and 3D mode is a confusing thing since you never have to consider such things in 2D), and extruded the angle to 5.75" long.

At first I was getting a lot of error messages about the model not being fully defined, but I figured out how to turn that off. I will have to come back later and figure that part out.

Then I discovered how to select a face on the part and rotate it normal so that I can sketch on it in sketch mode.

Other parts of the puzzle were solved when I found the "centerline" in the pulldown toolbar, and was able to use those as construction lines to lay out the work, similar to what one does with layout dye on a real part. I found the "snaps" toolbar, and that was a big help.

Part of the problem with the 3D programs is that they have so many toolbars and tool buttons it is not funny, and some work in 2D, and others work only in 3D, so you have to think in terms of two sets of toolbars, and remember which apply to what.

The constraints thing was throwing me for a loop also, and I must say me and constraints are not friends right now, but I am beginning to understand the importance and power of using constraints, but still learning those. Luckily, the constraints can be deleted if they get too pesky, and I figured out how to do that, but will have to be careful not to work against myself by deleting too many constraints.

Then I figured out you can change the color of an entire object, or just a single face of an object. That can be helpful when you are spinning the part around in 3D space, and need separate colors to keep track of which face you are on.

Another challenge is the fact that any sketch used to extrude into 3D has to be a fully closed figure. I generally draw cleanly enough for this not to be a problem, but the program does not tolerate any figure that is not closed with respect to extruding.

The "cut" feature was confusing, and I assumed (incorrectly) that any sketch used for cutting must also be a closed figure, but that is not the case as I accidentally and happily discovered. I forgot to include one of the 0.5" corner radius in part of the frame (you can see this in one of the screen shots, but luckiliy, I was able to use the "undo" feature to go back one step to the sketch I did for the side of the frame, and add that radius, and then run the "cut" command again.

The cut command can be used to bring a cut "through all" surfaces, or "up to a plane", or several other options which I am still learning.
You can also I think extrude or cut from the center of a plane equally in both directions, which I intend to use for cylinders to great advantage.

So while I have only made a simple part, I have made a quantum leap in getting a feel for what it is that I am trying to do with 3D.
Hopefully this will help some others with this conceptualization.

I have a handle on how to create 2D drawings from the model. In Solidworks, you just drag and drop the model into the basic 2D views, like front, side, top, isometric, etc. That is simple, but I am still figuring out how to get the dimensions to display properly in the 2D drawings.

My ultimate goal is to create an animated moving with a translucent cylinder so that I can see the engine running and look for interference problems.

Beyond that, I want to link in an Excel spreadsheet so that I can enter values in the spreadsheet and have the model change size accordingly.

Thanks again for the feedback. I think I am on a roll now with 3D.

Pat J

 

[JorgensenSteam]

Here is more of my second attempt at the frame.

 

[JorgensenSteam]

Here is more of my second attempt at the frame.

 

[JorgensenSteam]

Here is more of my second attempt at the frame.

 

[walnotr]

At first I was getting a lot of error messages about the model not being fully defined, but I figured out how to turn that off. I will have to come back later and figure that part out.

It is a good idea to try and fully define drawings as you go. It can make life simpler when and if you go back and modify the drawings. If a drawing is not fully defined, strange things can happen when you change an angle or dimension. It can be very frustrating at times and not always necessary, but as a rule you should work in that direction. Defining a drawing is not only accomplished by dimensions but also by "properties". i.e. vertical, horizontal, concentric, coincident, co-linear, and the like. Many of the properties are automatically selected for you as you create a drawing but are not always desirable. You may not want the center of an arc coincident to a line for example. All of these things can easily be changed once you find your way around and learn what works well for you when making your drawings. It is very helpful to look at drawings made by others to see how the have tackled a problem.

Steve C.

 

[imagineering]

You might find it helpful, (I'm assuming it works in Solidworks), to extrude to both sides of the Origin Plane.
ie; instead of a 100mm Extrusion being Z0 to +Z100, the Extrusion exists as -Z50 to +Z50.
This forces the Origin Plane to be in the Centre of your Extrusion, which is very helpful when laying out Sketches later on, as you now have a Centre Reference to work from/to.

Murray
(Inventor 2011 user).

 

[JorgensenSteam]

Thanks Steve and Murray, I will try those ideas.

Pat J

 

[Donrecardo]

At first I was getting a lot of error messages about the model not being fully defined, but I figured out how to turn that off. I will have to come back later and figure that part out.




My ultimate goal is to create an animated moving with a translucent cylinder so that I can see the engine running and look for interference problems.



Pat J

[/quote]

If you want it fully defined just go to the menus at the top and choose Tools/Dimensions/Fully define . It will pop up a window where you click on all entities in sketch and then click calculate, it will then fully define it for you.

As for looking into the engine to look for interference problems , rather than make it translucent , click on the section button and slice it on any plane , you will see all you want then

Don

 

[JorgensenSteam]

Thanks Don-

I will give those ideas a try.

Here is a quick drawing I made tonight for the frame.
2D drawings in Solidworks are created by opening a part file, and dragging and dropping on the 2D layout sheet. Each time you drag to a new position, you get a different view.

I guess this is where the power of 3D modeling begins to kick in.
It only took seconds to create this sheet, and any future changes I make to the model with be automatically updated in every view on every 2D sheet that I have created, and all the dimensions will also update automatically.

Now all I have to do is figure out how to get the dimensions on the 2D sheet.

Pat J

 

[Lockstocknbarrel]

Hi Pat
I had a play as well...................
Just love Solidworks went to Night School to learn.
If you want the file let me know.
What version are you running.
Kindest Regards
Beagles

 

[lee9966]

One thing I learned with SW is not to put too much in a single Sketch. Lots of sketches each determining a single feature makes it easier to work with for me.

For example if you have a surface that needs holes for mounting and holes for something else it is tempting to put all the holes into a single sketch. What I would do instead is to make one sketch for mounting holes, another sketch for the other holes.

Hope that helps, I am self taught an maybe others will correct me.

Lee

 

[JorgensenSteam]

I am going to revisit this post since I understand 3D modeling much better now than I did a year ago. These steps are generic, ie: they apply to pretty much any 3D program including Alibre.
This post was added on 3-26-12.

Lee has an excellent point, if you keep your sketches simple, then it is much easier to come back and correct a part of the design that may have a problem.

My approach to learning 3D was to purchase Alibre (I have Alibre and Solidworks), and just start the program and use it, since I have used 2D drawing programs for years.

So my problem was I would start Alibre, and then try and use it like a 2D drawing program. Big mistake, Alibre cannot be used in the same manner as a 2D drawing program, at least not if you plan on making 3D models.

A typical CAD 2D program has only one mode of operation, ie: you start the program and then draw on the screen using the mouse. What you see is what you get, and you can draw anything anywhere with impunity.

A 3D modeling program has two modes of operation, and you cannot do anything unless you understand what the two modes are, and when to use what mode. The two modes of a 3D program are "sketch" mode, and "modeling" mode (I think those are the correct terms).

Sketch mode is 2D drawing program, but you cannot use sketch mode exactly like you would use a 2D drawing program, I will explain why shortly.

Another big problem with 3D modeling is that you cannot use it without thinking about what you are going to do with it first. It would be like trying to machine an intricate part in the milling machine, and you put your part into the vise, start your mill, lower the bit into the work, and just hope something good happens. I can assure you nothing good will happen! You have to plan what you want to do first, such as define datum plane, define cuts, define the bits you want to use, shape of cuts, hole locations, fillets, etc.

So initially, I would open Alibre, try to draw something without a real concept of 3D, and then fail miserably. I did this for months.

So how do you get around the initial program shock?

My recommendation for an approach to 3D modeling is to start by visualizing the finished part that you are trying to model. Next, take that part, and slice it once like an orange, and look at the outline of the cut or section that is created. For an orange, a sectional view will look like a circle. So for 3D, you have to draw a circle, or for a sphere, actually a half-circe. You draw the half-circle in "sketch" mode on a 2D plane, and then revolve that sketch into a 3D sphere.

As you get into more complex shapes, it gets more confusing, and so you have to visualize breaking a part down into its basic geometric shapes. For example, a steam engine cylinder has the main cylinder containing the bore, the flanges on the ends of the cylinder, the steam chest, steam chest flange, valve face, ports and passages, counterbore, cylinder head holes, etc.

Start by figuring out what the single-most basic and fundamental shape of the part is. For a steam engine cylinder, that would be a cylindrical tube. So focus on creating a cylindrical tube first, and then adding additional features onto that tube.

You can make a 3D tube by just drawing a circle "in sketch mode", and extruding that shape into a solid tube at the length you want.